Magpie's Content
There have been 156 items by Magpie (Search limited from 27-April 23)
#39441 Powerful Aquarium Lighting
Posted by
on 16 November 2012 - 02:02 AM
in
General Discussion
Had a 5 minute look, I couldn't see any problems.
You could spend the rest of your life adjusting the silkscreen, it looks good enough.
Seeed has changed its ordering method, it is a bit more straight forward. Basically rename your drl file to .txt and zip it up.
I did Steff4 last night which just fixed the disaster that was steff3( where I didn't really look at the Gerbers). It was $32 10x10 posted. (Green, I have lost my confidence).
#39235 Powerful Aquarium Lighting
Posted by
on 13 November 2012 - 02:24 AM
in
General Discussion
PCB pre manufacture check list.
Done with Kicad and Seeed in mind but should be applicable to most boards.
TODO update as I think of more things to check.
SCHEMATIC:
schematic DRC passes ok.
FOOTPRINTS:
pcb foot prints are correct.
PCB:
design rules are set to match the manufacturer.
Current general settings:
Minimum value for tracks width: 0.2032 mm
Minimum value for vias diameter: 0.8890 mm
No microvias.
all tracks, set min clearance .2 if possible then .17 if possible otherwise .15 as absolute min.
do mount holes
do flooded zones.
add version and name of board.
add order number if necessary
add image?
add info to silkscreen for all connectors, but not underneath.
make sure silkscreen has orientation of all unipolar items.
check mechanical clearances
DRC passes.
in preferences->dimensions->pad mask clearance. set global solder mask 0.3mm for very small
check drill sizes are all standard (somehow)
PLOT:
probably turn component values off when generating gerbers.
dont invert y axis
Files:
.drl
Back.gbl
front.gtl
Mask_Back.gbs (dont confuse Mask with SolderPMask. (solder paste))_
Mask_Front.gts
SilkS_Back.gbo
SilkS_Front.gto
subtract silkscreen from mask
plot board outlines on layers
GERBERS:
Make sure all align.
Make sure zones don't flood kelvin connections.
make sure one via looks right.
make sure one through hole pin looks right.
make sure one top smd looks right.
look at the smallest smd.
check silkscreen isn't confusing and has all required details.
check each layer individually to make sure clearance is ok.
SENDING:
Add Readme.txt with order/quote number
Zip: 6 files + drill file + readme.txt
make sure that the board outline is in gerbers
#39224 Powerful Aquarium Lighting
Posted by
on 12 November 2012 - 11:29 PM
in
General Discussion
Have you assigned all nets to track types that have the min clearance of 0.2? Try and investigate one DRC error, you should be able to reduce it to 0 errors.
Recently I have only been using 1 track type, and assign every net to it. Then when I want to adjust the track or segment width I change the default width. It is because many of my tracks have different thicknesses. I go small as I approach the pins. I don't think this is how you are supposed to work, but it is quicker for me.
I made another mistake with my boards, I think I sent the solder paste mask instead of the solder mask. Who knows what will come back, but it will be wrong.
The solder paste mask is for making the stencils. Completely wrong. Fail. $50 dollars worth of Landfill.
I don't know if you can find a bigger chip that has so much ADC. 3 differential channels is pretty darn good for a 20 pin chip. Addressing them using spi wont be such a problem but there is a bit of code to write and debug.
Damp basement can probably be fixed with a fan or some fancy passive ventilation. If you can get the damp air out, you have a good chance. It iwll be good for the foundations to be a bit drier. Still it is a worry.
Let me check the gerbers before manufacture.
#39127 Powerful Aquarium Lighting
Posted by
on 12 November 2012 - 05:42 AM
in
General Discussion
Hi
I found and fixed a new problem. I am learning as I go, I just noticed this.
The problem is also on my expensive black boards for steff 3. damn it. Any work around I do is going to take a bit of work.
The problem is the flooded zone on the ground plane, floods the ground kelvin connection, thereby negating its kelviness.
I fixed it on your board by doing cutouts of the zones where it interferes with the kelvin connection.
Attached is the repaired board.
The Kelvin connection enables us to ADC some very low voltages. So it needs to be as noise and bias free as possible.
I have checked drc, It said some tracks were too close. I didn't change them I just set the DRC clearance of all tracks to 0.2mm from 0.25mm and everything passed. Seeed studio should be ok with a clearance of 6mil or 0.15mm.
the inductors seem to have the right footprint, they will solder fine.
Good luck with the house.
Attached Files
-
SteffNearlyFinished_fixedcutouts.zip 25.51KB
3 downloads
#38664 Powerful Aquarium Lighting
Posted by
on 07 November 2012 - 09:54 AM
in
General Discussion
here is a list of pcb manufacturers in ol' blighty
pcb manufacturers
Or probably go with seeed.
Try editing the yellow pcb outline layer, I just looked at your board there is loads of room, but you may just have to reduce the copper pour a fraction.
Just fit (edit) the pcb edges to be 50mm apart. and move the copper pour to be at least say 1mm away. Move the fiducials too or you can just delete them.
Or when you are completely done with the other stuff I can do this step for you. I gave it a quick test it took just a few minutes.
the price from seeed is going to be $US 35.00 and if you waste $15 on something you dont want then you get free postage. The have a resistor book 805, but at $60 it is very expensive.
when you order from seeed you are not paying for service so do everything they say and it will be ok. I forgot my order number on one board but it didn't matter it still came. This time I put it under a big inductor so no-one could see it.
pcb manufacturers
Or probably go with seeed.
Try editing the yellow pcb outline layer, I just looked at your board there is loads of room, but you may just have to reduce the copper pour a fraction.
Just fit (edit) the pcb edges to be 50mm apart. and move the copper pour to be at least say 1mm away. Move the fiducials too or you can just delete them.
Or when you are completely done with the other stuff I can do this step for you. I gave it a quick test it took just a few minutes.
the price from seeed is going to be $US 35.00 and if you waste $15 on something you dont want then you get free postage. The have a resistor book 805, but at $60 it is very expensive.
when you order from seeed you are not paying for service so do everything they say and it will be ok. I forgot my order number on one board but it didn't matter it still came. This time I put it under a big inductor so no-one could see it.
#38645 Powerful Aquarium Lighting
Posted by
on 06 November 2012 - 10:23 PM
in
General Discussion
Hi
I think you should build something soon, but I have a different idea for you for control.
the netduino can talk SPI and the attiny can talk SPI. so you could drop the tlc5940s completely.
Just have the netduino set the dimming level direct to the attiny via SPI. The only trouble with this is you would loose one channel of PWM, giving you two outputs per attiny.
Although if you can handle a small blink while the communication is done you could have 3 channels.
Also I have never written any SPI code in AVR so you would be on your own there.
L1 will be ok, it just needs to fit mechanically and I think it will fit but it will be tight.
If it doesn't fit you can easily make it fit by soldering L1 just off centre or filing a small notch into the ic socket.
You understand you need to use a socket dont you? I am not sure if I made this clear.
Right click on the footprint and Open the footprint in the module editor. Set the working library to say 'Andrew' and put all your mods as you do them in here. Create a new part from what is in the editor and save it into your footprint library. At this point you can save it as you make changes. Once it is done then delete the old footprints and place the new footprints into your pcb. The tracks may be no longer connected, so reconnect them using your knowledge of grids and snap to.
One day when I get something looking good made I will post about my latest version, hopefully soon.
If you get this first board made in small quanties, turn it on then I think you will find unexpected things, good and bad, especially in regards to the lighting aspect of it.
I think you should build something soon, but I have a different idea for you for control.
the netduino can talk SPI and the attiny can talk SPI. so you could drop the tlc5940s completely.
Just have the netduino set the dimming level direct to the attiny via SPI. The only trouble with this is you would loose one channel of PWM, giving you two outputs per attiny.
Although if you can handle a small blink while the communication is done you could have 3 channels.
Also I have never written any SPI code in AVR so you would be on your own there.
L1 will be ok, it just needs to fit mechanically and I think it will fit but it will be tight.
If it doesn't fit you can easily make it fit by soldering L1 just off centre or filing a small notch into the ic socket.
You understand you need to use a socket dont you? I am not sure if I made this clear.
I tried editing the pad offset, but every time I pressed OK, and went back in to the settings, it had gone back to zero?
Right click on the footprint and Open the footprint in the module editor. Set the working library to say 'Andrew' and put all your mods as you do them in here. Create a new part from what is in the editor and save it into your footprint library. At this point you can save it as you make changes. Once it is done then delete the old footprints and place the new footprints into your pcb. The tracks may be no longer connected, so reconnect them using your knowledge of grids and snap to.
One day when I get something looking good made I will post about my latest version, hopefully soon.
Yes I think before the final board is built you could optimise, but it is so hard to get the perfect design from scratch. It is iterative and I think 2 iterations will be your minimum.Let me know how you get on with your new boards, out of interest I know you have dropped a channel, but how small do you think I could realistically drop these boards to? I don't know if I definitely will, especially if these boards work, but I may lay it all out on one big board eventually with the TLC board built in and the power distribution for the 30 channels will be much more elegant and a lot of the connectors could be dropped. I could essentially get away with a GO! bus connector and a power plug, but this really is dreaming ahead!
If you get this first board made in small quanties, turn it on then I think you will find unexpected things, good and bad, especially in regards to the lighting aspect of it.
#38545 Powerful Aquarium Lighting
Posted by
on 05 November 2012 - 09:56 AM
in
General Discussion
Hi
edit: sorry I probably wrecked the kelvin connections
I did fix it up.
I emailed you the brd and the gerbers. to save on my upload space.
The problem was a few unconnected tracks that were actually connected but the DRC isn't smart enough to realise.
there was only 3 but the the DRC thought there was heaps.
The problems (gotchas would be more accurate) were caused by the grid settings, nets wont be connected unless they snap to the grid. if you change grid settings some of your pads will no longer snap. Also Kicad doesn't seem to remember your grid settings so you have to change it whenever you open up. Try to use the same one or two all the time. I had to go down to the very lowest to get one track to snap.
The other problem is not actually a problem with the board but with Kicad. the DRC doesn't understand the copper areas and that everything inside is connected. So work around this I just join the unconnected ground pins on the underside of the board with thin tracks until the DRC says no errors. The actual copper pattern ends up being the same.
Its like programming, get rid of the warnings so you can see important ones when they eventuate.
Also a put vias into a lot of the ground pads, which I have only just learned how to do.
Apparently my steff3, 2 channel, 36 volt, Black boards are finished manufacture and are returning to me.
#38474 Powerful Aquarium Lighting
Posted by
on 03 November 2012 - 11:47 PM
in
General Discussion
If you edit the pad in the component editor it gives you the offset x and y and the size x and y of the pad. I found editing these text boxes to be the easiest method.
The hardest bit is saving it into the correct library and loading the module back into the board, which you have done.
I dont know if the inductors are any good. The bigger the inductor the less heat and higher efficiency, but higher cost and space, you have to weigh it up. Make sure it has a saturation current of at least 2amps.
I managed to clear up all my errors, do you have an unconnected track? If you do the location of it will probably not be where you expect because the software doesn't know where exactly the net is separated, because it is separated everywhere.
If you want I can probably fix it for you, but I need a zip with all main files + any special libraries and modules.
Take your time buying your house, a bargain will come along.
#38421 Powerful Aquarium Lighting
Posted by
on 03 November 2012 - 11:47 AM
in
General Discussion
I think they will solder alright, it is just that if the pads are too big they may short out through the iron shield.
But if you just put a tiny square of insulator underneath, you can solder on both legs any way. It's a bit of a bodge but will work if the footprint is wrong.
Does that mean you've been drinking for 12 hours? Don't fall in the aquarium, I am picturing some sort of James Bond evil villain type of aquarium.
what those atlas guys say about remote monitoring, is so true.
But if you just put a tiny square of insulator underneath, you can solder on both legs any way. It's a bit of a bodge but will work if the footprint is wrong.
Just going to few about 12 house now, what a Saturday! But I will make the amends and catch up later.
Does that mean you've been drinking for 12 hours? Don't fall in the aquarium, I am picturing some sort of James Bond evil villain type of aquarium.
what those atlas guys say about remote monitoring, is so true.
#38363 Powerful Aquarium Lighting
Posted by
on 01 November 2012 - 11:56 PM
in
General Discussion
I thing I found useful was a SMD resistor and capacitor book. It cost about $35 from Ladyada I think, but many people sell them, they hava all SM805 foot prints in useful ranges.
I will look when I get the chance.
I have finally convinced my boss to let me design a board for work. Solar battery charger just 20W. I better not stuff it up.
He wants me to use MyroPCB, they do a fair bit of manufacture for us.
I am not sure, if they will fit, as there is no footprint. If it is metal under those inductors then you will have to watch for shorting via the inductor sheild if the pads dont fit properly. But if the boards came back and were wrong it wouldn't be such a problem as you could put down the flimsiest layer of plastic or paper to insulate this and then solder around it.
the little inductor under the ic might need to move closer to the edge, maybe half a pin pitch. just so it doesn't get blocked by the ic socket.
I would put + and - on the silkscreen top layer for each connector. but outside of the footprint so that you can easily work out +- when you are plugging. Use the text tool in Kicad.
#38267 Powerful Aquarium Lighting
Posted by
on 30 October 2012 - 11:41 PM
in
General Discussion
It is hard not to make a mistake on a board. You will definitely see improvements you will want.I added some drill holes, I will probably relay the board slightly once I have tested one working.
the Gerber lines up properly, I don't know about the .pho file.
Just make sure the foot prints of the stuff you order matches the ones on your board.
In steff2 I ordered D2Pak fets but had footprints for DPak fets luckily this mistake wasn't critical as I could force them on.
If you want to use Seeed Studio then I would scrape off approximately 1.1mm of the height of your board. It will save you money.
If you use someone else it may not matter.
Height : 30.4 -> 82.5 = 51.1mm
Width: 123.2 -> 261.6 = 138.4mm
Seeed Studio use 50mm increments for pricing.
In kicad there is a yellow pcb edge layer, right click on the lines and edit the y value to make it 50mm long.
Follow the instructions from Seeed Studio to the letter, for you first spin use green it is cheaper.
If you cut the board down to 50mm x 138mm then you can buy the 5cm x 15cm option from seeed.
PCB Cart is another place.
But I think UK has a lot of manufacturers too.
#38215 Powerful Aquarium Lighting
Posted by
on 30 October 2012 - 01:42 AM
in
General Discussion
thats an important cap. the digikey part will be fine.
The only two sizes I used are 805 and 1206 so the big ones are 1206. I think all the caps are 805 but the resistors are mostly 1206. the 0.1ohm are 1206 I think.
different board houses have different ordering requirements I have been using Seeed Studio (very very cheap but they have a few hoops to jump through).
Make sure after plotting you view in Gerber viewer.
It should be 6 layers + the drill file. Put them all in the gerber veiwer together and check alignment of the holes and tracks. Make sure everything sits on top of one another.
the layers are.
Copper top and bottom
solder mask top and bottom. this layor covers most of the board except where you need to solder.
silkscreen top and bottom.
To plot gerbers press plot and use defaults. There is a tute on this out there. Basically I just use defaults. Dont invert the Y axis. Also put the board edges onto the plots.
plotting is actually quite easy.
I just sent off steff3 to Seeed. ( 2channels, 36V, 100mm x 50mm board, black) Hopefully this is the One. Steff2 was too big and too green. Hard to put into a light fitting.
Edit : oh and dont forget to put mount holes in, like they did with raspberry pi. I use a model called '1pin' which has a drill hole of 1/8 inch.
This will let you use 3mm screws and rivets.
#37736 Powerful Aquarium Lighting
Posted by
on 21 October 2012 - 11:09 PM
in
General Discussion
Last time I used Seeed Studio but they do boards in certain sizes which may not fit your board.
They do boards in multiples of 5cm dimensions. See what fits! They are a truly minimilist service.
The advantage of these guys is they are super cheap. 10 boards for $50 or something.
itead is the other very cheap one.
I also used Olimex? Bulgaria. They were good and but a bit more expensive, but based in Europe so may be faster. (Actually they have suspended their service because they are at full capacity.) So much for the Euro zone economic calamity.
You could try Fritzing and just get one board done and see if it works.
Take some time to get the silkscreen right, it makes soldering much easier.
Also dont expect zero mistakes first board, aim for no critical mistakes.
I haven't really done much layout so I am learning too. But trying to explain the Kelvin connections to someone is hard, so I thought I would just do them.
#37418 Powerful Aquarium Lighting
Posted by
on 19 October 2012 - 08:48 AM
in
General Discussion
Fixed 5 volts as best I could, still needs mount holes.
Attached Files
-
steff35v.zip 44KB
6 downloads
#37401 Powerful Aquarium Lighting
Posted by
on 18 October 2012 - 10:03 PM
in
General Discussion
I just remembered, I didn't put in any drill holes for mounting.
And I made a mistake with the 5v rail.
I will redo the 5v, it should fork at the bulk capacitor with one trace going to the attiny and the other trace going everywhere else. This should give better noise immunity.
I think I prefer the 12volt version though. Noise may be a problem with the 5v version, it is hard to say. Although I think you are using the internally regulated reference for the ADC so it might be ok. The 12v version gets 5 volts by using a linear regulator, this give it a very clean 5v. Whereas the 5v rail in your circuit has noise from the switching of the Fets straight onto it.
#37372 Powerful Aquarium Lighting
Posted by
on 18 October 2012 - 08:13 AM
in
General Discussion
Hi
I laid it out for you, but bear in mind I didn't do any checking, so please check all, I take no responsibility. there is always a stuff up or 7.
though it passed DRC.
I didn't knowingly change the schematic. Or the models used.
I am getting better at Kicad even the fill areas are getting easier, but as you know there are quite a few strange things in Kicad.
I thought rather than explaining again I would just do it. If you want to change things around, please do.
I may have put things too close, please check, I kept the same size board as you, but the connectors are in different spots.
I removed the zip I fixed it up a bit.
#36036 Powerful Aquarium Lighting
Posted by
on 26 September 2012 - 11:11 PM
in
General Discussion
No worries about helping, I know many many projects die a death and I don't want your project to die because of me pulling out, and advising you what to do is easier than doing anything myself.
Sailing to work are you serious?
I really thought you could almost copy my layout of the output stage. Assuming your connector requirements aren't too different.
So layout the power stage first for one channel, including 2 x bjt and the sense resistors. With the best track widths, try to keep on one side if possible but use the 2nd layer for short runs if you need it.. Get this section laid out perfectly. Keep all the components close as is comfortable.
If you want I can check at this stage, before you go further. I have a notification on this thread.
Delete the components for the other two channels from the pcb editor.
Then cut and paste the perfect layout to make 3 copies.
then edit the component identifiers to connect the copied channels to the ratsnest.
This should give the three channels fully connected to everything else in the same channel.
After this layout the attiny and the caps and resistors, you could almost copy my layout. The only change I would make is the smd inductor I would put it on the top layer with the IC socket( use a socket). It should fit in mechanically, within the socket. Once you have these sorted and close to the attiny.
give me another look.
Lastly you need to route the pwm outputs and the current sense inputs. The Kelvin connections from the sense resistors are the thin 2/3 tracks together. Dont use vias on the Kelvin connections. Use Vias only where you really need to(which you will) firstly on the power and then the second preference is the the pwm.
The kelvin connections only have less than 100mV max, and we are trying to detect changes in the micro volts. They are run together so that any noise present will effect each track similarly.
#35937 Powerful Aquarium Lighting
Posted by
on 25 September 2012 - 02:16 AM
in
General Discussion
I have done, I found it quicker now that I know what I am trying to acheive. If you had a lot of obvious connections then I think that the autoroute can do those fairly easily.I've been playing around trying to do the track widths, do you place all the tracks yourself
The ratsnest will dissappear as each node is fully connected. If you are using vias for higher current paths then you can use multiple.and if so how do you make sure you are connecting up correctly/ deal with vias?
Default for thin, 8mm for thick and say 3mm if it is carrying some current. But reduce these widths just for segments where it is necessary.What widths do you think I should be aiming for, for my thin, medium and thick traces and what clearances would I need?
Do your placement first obviously.
I haven't looked have you changed anything since last time I looked?In terms of my layout, which is similar(ish) to yours can you see anything that will/may cause me a glaring issue?
Sorry Andrew, I was actually Sailing all weekend, it was fantastic.
Did you sort out how to change track widths, I know it is very cumbersome.
You probably found this out already but
assign a track to a track type in the digital rules.
When you lay it out it will take the track width of the track type.
If you want to temporarily make some tracks a different width such as for the ground plane, Where the Kelvin connections carry a tiny current and the power ground has high current you can just change the track width for the track type(eg. High Current) while you lay that track. Then set it back to normal.
Also sometime you want to run the track thin into the pins but run it fat for most of the length.
First run it thin, then change the track thickness for the track type and right click and adjust the track thickness on the segments that you want thicker.
for the thicknesses
Connections into the processor only need to be thin. Power tracks make thick. Tracks on the ouput stage make thick as you can but thin them down as they feed into the component legs. It basically comes down to the current through the track. 8mm wouldn't be amiss joining the inductor to the Fet and the diode, if you can fit that much.
I quite liked my posistioning of the components, to minimise track lengths for the high current tracks. But maybe you want the connectors to be organised differently.
As for the Kelvin connections run them as pairs or threes lik it did. The only place the ground of the kelvin connection touches ground is at the sense resistor.
the point is we want to measure the voltage of the ground at the sense resistor compared to ground at the micro, but using only the minimum current we can to do it. (Conceptually tricky). Also we want the minimum induced noise so we run the differential inputs right next to each other, for as long as posible.
Hope this helps
#35299 Powerful Aquarium Lighting
Posted by
on 15 September 2012 - 01:12 PM
in
General Discussion
Hi
You have managed a lot of the hard stuff, ie working with PCB layout is hard.
Did you use autoroute? Looks a bit that way.
The most obvious problem is the track widths. on the high current paths.
Also C1 pin 2 is not connected.
I think you could virtually copy my layout, apart from the step up transistors of course.
Apparently component placement is the key to pcb design.
In your Design rules you have only small track widths even for the power tracks.
Also the kelvin connections aren't done. You are just sharing the ground plane.
These are hard to explain,
Technically the Gnd side of the sense resistors are shorted to earth. But the trick is that no short is a complete 0 milliohm.
So for each sense resistor short the ground pin to the ground plane but as well run a pair of tracks to the attiny filter input circuit( 10k and 100nF) , Right next to each other one from each side of the sense resistors. These tracks only go to the filter they do not touch ground except at the sense resistor. Have a look at my layout it might be clearer.
the idea is that only current that is required to measure the voltage travels along these tracks, and the loop area of the pair of tracks is minimised.
I can try and explain again if you need but look up Kelvin connections if you have any doubt.
You will make mistakes in the design but often they can be fixed with a cut and a join. My Fets had the wrong foot print, I incorrectly chose a smaller one but it wasn't a show stopper.
The rest of my foot prints were right.
#34664 Powerful Aquarium Lighting
Posted by
on 04 September 2012 - 11:18 PM
in
General Discussion
Hi
I've been a bit preoccuppied too.
Also I'm actually having trouble with the mechanical and light aspects of my light fittings.
I would keep the little drivers as functional blocks and close together.
ie. inductor, diode, fet, connector, sense resistor, and then the bjts and other resistors.
Once you have perfected this as a block. I would copy it and manually assign the part id to each of the new parts.
Once you do this the little node lines should dissappear to show that it matches your schematic.
this should give you a perfect copy of part of your circuit but with different part ids.
Do you use source control? I really consider it a must.
If you do you can to the diff between your original file and your new file.
For doing this sort of copying work, It might actually be easier to edit the pcb as a text file than in the pcb editor. Look into it. It will give you real insights into what the pcb editor does.
You are probably having trouble changing track widths because you have DRC on and so all tracks will go to the default track width.
In DRC I think you need set track widths for each node.
create 3 types of track/node.
I use thin, normal and thick.
Set each of them to the thickness you want.
The assign all nodes to the appropriate type of track.
When you go to place a track it will select the correct thickness.
The only trouble is making the super thick nodes go into a small pin.
Here you temporarily change the thickness of the track type. -> lay the track -> reset back to the normal thickness.
Flooding areas was a bit weird, I only recently worked it out, I cant remember off the top of my head though.
You can leave it to last anyway.
When I get the chance I will have a look.
I would use Seeed Studio because they are sooo cheap but the turn around is a bit longer.
Just keep each channel as a small perfected block and you should be able to move them around quite easily.
I am going long and thin and black for the next spin of my board.
I want to make it look a bit Steam Punk, so I can expose part of the board.
#33122 Powerful Aquarium Lighting
Posted by
on 04 August 2012 - 11:58 PM
in
General Discussion
Hi
Just to start by giving everything standard footprints. Doesn't matter if the footprints are wrong as long as the pins are the same.
Then in pcb editor right click and edit module on the components that need changing. Then on each pin you can edit by right clicking. The pads are normally simple shapes, so you can edit the them by just changing the sizes and offsets in the text boxes.
If you need a complicated pad shape you can make it as two or more separate pins but give them the same pin number. This is a strange but necessary work around and it does work fine.
Work out how to save these modified mods into your own mod library and then associate them.
Did you see a youtube video on Kicad, I found one in particular it quite useful.
the footprints for the caps don't need to be exact, if it roughly good enough it should solder ok, you are better off using a standard footprint because you might change caps anyway.
Also there is a difference on components between the actual footprint and the solder pad needed. the solder pad is normally a bit bigger around the edges of the component so you can stick the point of the soldering iron onto the pad itself.
ps. the reason I chose 4.7uF through hole is because I had 100 of them already.
Firstly, put your Kicad stuff including libs and mods into source control, if you are going to work effectively this is a must, being a programmer you probably already use source control, it is so easy to make a mistake by clicking the wrong button, that rollback will save you and give you clues into how it all works and tell you what has been changed.There are foot prints for this type of cap but none that are exact so I wanted to edit the component to make one for my cap, but couldn't workout how to do this in the editor. The lines didn't seem selectable and the couple of pdfs I read didn't seem to help much either?
Just to start by giving everything standard footprints. Doesn't matter if the footprints are wrong as long as the pins are the same.
Then in pcb editor right click and edit module on the components that need changing. Then on each pin you can edit by right clicking. The pads are normally simple shapes, so you can edit the them by just changing the sizes and offsets in the text boxes.
If you need a complicated pad shape you can make it as two or more separate pins but give them the same pin number. This is a strange but necessary work around and it does work fine.
Work out how to save these modified mods into your own mod library and then associate them.
Did you see a youtube video on Kicad, I found one in particular it quite useful.
the footprints for the caps don't need to be exact, if it roughly good enough it should solder ok, you are better off using a standard footprint because you might change caps anyway.
Also there is a difference on components between the actual footprint and the solder pad needed. the solder pad is normally a bit bigger around the edges of the component so you can stick the point of the soldering iron onto the pad itself.
that's what I did, the caps need to be close to the processor and the resistors are not so critical. I would go with that unless you have a specific reason. The bigger components are easier to work with.Am I right in saying all the resistors should 1206 and all the other caps should be 0805?
ps. the reason I chose 4.7uF through hole is because I had 100 of them already.
#33111 Powerful Aquarium Lighting
Posted by
on 04 August 2012 - 12:15 PM
in
General Discussion
I just checked the channel independence and all is good. No visible effects of one channel effecting another.
I did an efficiency check 3 channels at 20.5 volts input and 1.23 amps input gives 25.2 watts.
V1 20.27v I1 430mA p1 8.72W (not actually switching, because it is turned fully on)
V2 20.3v I2 350mA P2 7.11W (barely switching)
V3 17.56v I3 440mA P3 7,73W (only 6 leds in series not 7 that is why it is different)
Pout 23.56W
efficiency 93.5 %
Obviously this figure has some error, but very hard to say what it is, but I think 93.5 % is in the ball park, nothing is dissipating heat bar the leds.
Theoretically when the channel is fully on I will get losses in the inductor 40mOhm and the sense resistor 100mOhm and Rds 40mOhm.
At 440mA this should give me a voltage drop of 0.0792 volts coming from 24 volts which is 99% - minus the gate drivers.
Still I wanted over 90% and I am sure I have that.
the light seems very solid now it's been running for hours, cant fault it at the moment.
#32993 Powerful Aquarium Lighting
Posted by
on 02 August 2012 - 01:51 AM
in
General Discussion
Hi Andrew
Good news
I have fixed the init problem by setting the brown out fuse to 4.3 volts.
I have three channels current sensing. Controlled by the dimmer.
the differential sensing works and so I can just touch the slider and the output will correspondingly change, the output is quite stable.
I will do more accurate tests later.
All channels are behaving the same way.
I have almost no flickering, maybe the tiniest bit at very low light settings.
I have tons of scope to tighten the feedback loop, this will be the major factor of any flickering.
I have written it in C. But have been told that assembler is better for this job.
I am using Amtel Studio 6, which should be familiar if you us a netduino.
I will give you the project now but I will probably change things before you are ready to program.
the only thing not planned is I am using the 2.56 vref for the dimmer as well as the current sense.
there is a good chance it will work with 5v as planned.
Also I don't think we need Attiny461a as the code and ram requirements are very small, you can probably save your cents and get the 261a instead.
I can give you help in the layout. not that I am an expert I've only done 3 boards but no abject failures yet. Apart from the silkscreen layers.
Have you sorted out your tlc5940 stuff yet?
NB I haven't tested the 3 channels independently yet, I am worried the current sense may be subject to cross talk, hence the strange track layout.
Attached Files
-
Steff2AS6.zip 51.7KB
1 downloads
#32978 Powerful Aquarium Lighting
Posted by
on 01 August 2012 - 01:29 PM
in
General Discussion
they seemed to be $6.00 each or was that a pack of something.Found these they seem relatively cheap and available what do you think?
Try PCE3340CT-ND I think you should be able to get something for around 50 cents, you can probably go smaller 33uF on these if you want.
from memory it is in devices and called cp1In terms of the cap symbol, which library do I need to look in?
Also you mentioned in terms of the library that I may need some files? Do you think this is the case and is this for the PCB design as opposed to the actual schematic?
more so in pcb editor, these is an excellent pdf that is built into the toolbar on pcbeditor. use that to help find footprint names
I have the channels 1 and 2 current sensing and stable.
Now I have init/boot problems and channel 3 I cannot get to current sense.
#32960 Powerful Aquarium Lighting
Posted by
on 31 July 2012 - 11:44 PM
in
General Discussion
This is just a bypass capacitor for the whole board. It's size depends on the power used by the board and the length of wire to to power supply and the power of your power supply.C21 larger electrolytic capacitor of 50uF, I have been unable to find a suitable part even in stock on digikey, am I missing something or is this a fairly heavty cap? Can you suggest any examples any where?
Anything from 10uF to 220uF would be fine, I suggest 50uF but it wont make a difference.
Also its voltage rating doesn't need any high voltage either. 16v is fine but 25v is good too. Remeber it is electrolytic not ceramic. For a computer analogy, the ceramic is like your ram and the electrolytic is like your hard drive. They are often in parrallel. It should be easy to find. The pdf schematic component is wrong is should show a curve on one of the plates and a plus sign. They are unipolar and need to be orientated correctly.
Yes that is fine.Almost there with the schematic, although I have just been changing the values of the components is this ok?
The diagram looks good otherwise,
dont worry about the DRC on those last things, you can safely ignore it.
If you really want to fix it you can edit the module and then edit the pins to be power in or whatever satisfies DRC.
Both of those are standard (12 mils x 6 mils) and (8mils x 5mils) dimensions with mils being 1 thousandth of an inch.On the topic of foot prints is there a standard for all the resistors I remember you mentioning an issue you had 0805 and 1206 I think?
Don't go any smaller than 0805 and I would use 1206 out of choice as it will be easier to measure and fix. I used 805 on the caps so I could fit them in nice and close to the ATTiny,
and 1206 on most of the resistors. When buying another thing to watch is the tolerance, but in this case it doesn't matter too much. Though it is easy to get 10% on ceramic caps and 1% on resistors so I wouldn't settle for less, incase you have spare and want to use them on another job.
After that I reckon you are done.
Now assign and/or make footprints and do the pcb layout. I find there is a fair bit of back and forth between metric and imperial while I do and check foot prints.
But I still haven't got the firmware to do the differential ADC inputs, with the 32 x Gain,
I have measured current but only as a one sided input, and because you get no gain I only get a tiny voltage.
I will try again tonight. My feeling is that it should work so it is only a matter of time.
